CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   I really need some help on this problem (http://www.cfd-online.com/Forums/star-ccm/112217-i-really-need-some-help-problem.html)

htwana January 23, 2013 22:47

I really need some help on this problem
 
1 Attachment(s)
Hi everyone,
I am trying to simulate the heat transfer performance of supercritical water flow in vertical upward round tube with 3.2 mm diameter. Here is a problem that bothers me for long time.
The distribution patterns of the calculated wall temperature and heat transfer coefficient are not reasonable. The wall temperature increases too fast near the inlet of the tube and then increases almost linearly along the length of the tube. Since the coolant temperature increases almost lnearly along the length of the tube, the heat transfer coefficint, which is defined as
h=q/T, decrease very fast near the inlet of the tube and then almost keeps constant.

I can not find the reason why the wall temperature increases so fast near the inlet of the tube. It should increase step by step, and the difference between the wall temperature and coolant temperature should increase with the increasing of the coolant temperature.

I tried several other k-e models. I got similar unreasonable distribution patterns.
I attached a figure of the distributions of the temperature and heat transfer coefficient.
Would some one please tell me what possible reasons can cause such problem?
Thank you all, thank you for your kind advise

siara817 January 24, 2013 03:41

Can you explain what is the coolant here?

htwana January 24, 2013 03:44

I am sorry that I didn't describe clearly. The coolant is supercritical water. The temperature of coolant is higher than 390 oC

Pauli January 24, 2013 12:16

Not knowing your geometry, consider this more an interpretation of the graph you shared.

The graph indicates the entrance (length < 0.1m) has a much higher heat transfer coefficient than the remainder of the tube. This is driving the computed temperatures. The question is why does the entrance have higher heat transfer coefficient.

From a flow physics standpoint, my initial assumption would be entrance effects (separation & mixing) cause additional mixing (varying velocity profile). At length > 0.1 the flow is fully developed. This provides a constant velocity profile & the h=q/dt relationship you expect.

From a numerical calculation standpoint, you should be asking questions regarding how the heat transfer coefficient is calculated. Are you using wall functions or resolving the boundary layer? Is grid resolution adequate? Etc, etc. Computing heat transfer coefficients under pipe entrance conditions is not wall functions strength.

Prashanth.A January 24, 2013 13:26

Could you put up a schematic of the model you are working with, I have worked with numerically modeling similar flows (multi-phase flows, lot of empiricism). I have got results which are analogous to yours, I was working on Micro-Processor Cooling Techniques, Which is reversal of your application.

htwana January 24, 2013 21:06

all informations of my simulation-1
 
The geometry is very simple. The length of tube is 500 mm. The diameter is 3.2mm. There is no wall thickness, and we only consider the fluid region. The uniform heat flux is 800kW/m2, the mass velocity is 1000kg/m2s , the temperature of inlet is 670 K and the pressure at outlet is 25 MPa. Flow direction is upward.

htwana January 24, 2013 21:07

all informations of my simulation-2
 
1. The needed thermal properties of water are as follow:


density
Number of interval
3
Interval ranges
[663,700, 800, 1073]
Numbers of coefficients
[5,5,4]
Coefficient
[20888437.32897, -121466.279457929, 264.892650225018, -0.2567597311521, 0.000093333082540744, 79195.9972248006, -404.619712014594, 0.7784131025619, -0.00066713291581415, 2.1477224361164E-07, 902.76678358608, -2.2681931455009, 0.002078145302, -6.5474813334491E-07]
Exponents
[0.0,1.0,2.0,3.0,4.0, 0.0,1.0,2.0,3.0,4.0, 0.0,1.0,2.0,3.0]
--------------------------------------------------------------------------------
Specific heat
Number of interval
3
Interval ranges
[663,683,783, 1073]
Numbers of coefficients
[5,5,5]
Coefficient
[72098255169.205, -426901983.90771, 947913.913893974, -935.475678541713, 0.3462040914552, 35740652.493319, -189447.825833259, 376.86407580743, -0.3333750897413, 0.00011063602503477, 223117.120300903, -870.188643358111, 1.2944485418665, -0.00085908519886809, 2.1442187362133E-07]
Exponents
[0.0, 1.0, 2.0, 3.0, 4.0, 0.0, 1.0, 2.0, 3.0, 4.0, 0.0, 1.0, 2.0, 3.0, 4.0]
----------------------------------------------------------------------------------------------------------------------
Dynamic viscosity
($Temperature<663.0)? 3.15716e-5:
(($Temperature<683.0)? 6.9224264624736-0.0408832952645*$Temperature +0.000090549079244015* pow($Temperature,2)-8.913669797436E-08* pow($Temperature,3)+3.2906108603975E-11* pow($Temperature,4):
(($Temperature<783.0)? 0.0108989512696-0.000057839685831513*$Temperature +1.1532390544032E-07* pow($Temperature,2)-1.0216997356426E-10* pow($Temperature,3)+3.3955858119227E-14* pow($Temperature,4):
(($Temperature<1073.0)? -0.0000032427270621927+4.741942361337E-08*$Temperature +-4.78555217991E-12* pow($Temperature,2): 4.21E-5)))
-------------------------------------------------------------------------------------------------------------------------
Thermal conductivity
($Temperature<663.0)? 0.2264:
(($Temperature<695.0)? 47661.033038555-278.416789654012*$Temperature +0.6099315425136* pow($Temperature,2)-0.00059388587645495* pow($Temperature,3)+2.1685650279812E-07* pow($Temperature,4)
:
(($Temperature<775.0)? 185.834410219319-0.9793944425447*$Temperature +0.0019389248748* pow($Temperature,2)-0.0000017078378939546* pow($Temperature,3)+5.6465757723963E-10* pow($Temperature,4):
(($Temperature<1073.0)? 2.4199512766181-0.0094779285294*$Temperature +0.000014350317833471* pow($Temperature,2)-9.5997271574745E-09* pow($Temperature,3)+2.421812079001E-12* pow($Temperature,4): 0.123)))
------------------------------------------------------------------------------------------------------------------------
Prantl Number
($Temperature<663.0)? 3.9489:
(($Temperature<700.0)? 712655.370282141-4137.78650804068*$Temperature +9.0095886619281* pow($Temperature,2)-0.0087191263008* pow($Temperature,3)+0.0000031643427014962* pow($Temperature,4):
(($Temperature<800.0)? 1789.0113166512-9.1712038684109*$Temperature +0.017667884118* pow($Temperature,2) -0.00001514546110914* pow($Temperature,3)+4.8732160696751E-09* pow($Temperature,4):
(($Temperature<1073.0)? 35.1933611129059-0.132228857307*$Temperature +0.00019253019932984* pow($Temperature,2)-1.2511500694886E-07* pow($Temperature,3)+3.0554723673796E-11* pow($Temperature,4): 0.91)))

htwana January 24, 2013 21:10

all informations of my simulation-3
 
1 Attachment(s)
2. The generated mesh is shown in Fig.1.

htwana January 24, 2013 21:12

all informations of my simulation-4
 
1 Attachment(s)
3. The selected physical model

htwana January 24, 2013 21:16

all informations of my simulation-5
 
1 Attachment(s)
4. the wall y+ is from 16 to 33

htwana January 24, 2013 21:21

all informations of my simulation-6
 
1 Attachment(s)
There are totally three boundaries: Inlet Outlet and wall

htwana January 24, 2013 21:24

all informations of my simulation-7
 
1 Attachment(s)
A line-probe is generated on the wall boundary to be used to get the wall temperature.
Nine plane sections are generated along Z direction to get coolant temperature by using Surface Average of the Reports

htwana January 24, 2013 21:37

Quote:

Originally Posted by Prashanth.A (Post 403836)
Could you put up a schematic of the model you are working with, I have worked with numerically modeling similar flows (multi-phase flows, lot of empiricism). I have got results which are analogous to yours, I was working on Micro-Processor Cooling Techniques, Which is reversal of your application.

All informations have been uploaded. As my understanding, you use coolant to cool the micro-processor, right?

htwana January 24, 2013 22:14

Quote:

Originally Posted by Pauli (Post 403819)
Not knowing your geometry, consider this more an interpretation of the graph you shared.

The graph indicates the entrance (length < 0.1m) has a much higher heat transfer coefficient than the remainder of the tube. This is driving the computed temperatures. The question is why does the entrance have higher heat transfer coefficient.

From a flow physics standpoint, my initial assumption would be entrance effects (separation & mixing) cause additional mixing (varying velocity profile). At length > 0.1 the flow is fully developed. This provides a constant velocity profile & the h=q/dt relationship you expect.

From a numerical calculation standpoint, you should be asking questions regarding how the heat transfer coefficient is calculated. Are you using wall functions or resolving the boundary layer? Is grid resolution adequate? Etc, etc. Computing heat transfer coefficients under pipe entrance conditions is not wall functions strength.

Thank you very much for your kind, patient analysis.
I can understand the entrance effect at length < 0.1 m. But the wall temperature distribution pattern is more like a simulation result with constant thermal properities, not with changed thermal properities.
In fact, in the high enthalpy region of supercritical water, all thermal properties of water are functions of coolant temperature. I defined all these thermal properties using field function of STAR CCM, or polynomial density and specific heat.

I attached all informations used in my simulation. Are there any important steps that I missed during the simulation process?

Thank you very much anyway!

Pauli January 25, 2013 01:03

Did you use a uniform inlet velocity profile? Or did you apply a parabolic profile representing fully developed flow? From the information you provided, it appears you specified a uniform profile. I believe that is the primary source of your high h at the inlet.

Your setup panel shows you chose a 2-layer all y+ wall treatment. The y+ plot shows your y-plus is in the range where wall functions are used. With wall functions, the heat transfer function coefficient is strongly driven by the near wall velocity.

Your mesh & y+ values are nice. I'm guessing the red spot in the y+ plot is the inlet. That observation coupled with your setup panel led me to believe you have a uniform inlet velocity profile.

htwana January 25, 2013 01:31

Quote:

Originally Posted by Pauli (Post 403927)
Did you use a uniform inlet velocity profile? Or did you apply a parabolic profile representing fully developed flow? From the information you provided, it appears you specified a uniform profile. I believe that is the primary source of your high h at the inlet.

Your setup panel shows you chose a 2-layer all y+ wall treatment. The y+ plot shows your y-plus is in the range where wall functions are used. With wall functions, the heat transfer function coefficient is strongly driven by the near wall velocity.

Your mesh & y+ values are nice. I'm guessing the red spot in the y+ plot is the inlet. That observation coupled with your setup panel led me to believe you have a uniform inlet velocity profile.

Thank you very much for your help.
I did use uniform inlet velocity profile in my simulation.
The problem of my simulation is that the simulation results are more like we use constant thermal properties, rather than changed thermal properties.
I have defined all thermal properities as the functions of the coolant temperature. But it seems all these functions are not rightly used.
I don't know what causes this problem

Prashanth.A January 27, 2013 10:54

In the Physics model, change the fluid setting from Liquid (H2o) to Multiphase Mixture with inlet being only Liquid H2o. That should solve the problem if there was any.

htwana January 30, 2013 04:12

1 Attachment(s)
Quote:

Originally Posted by Prashanth.A (Post 404330)
In the Physics model, change the fluid setting from Liquid (H2o) to Multiphase Mixture with inlet being only Liquid H2o. That should solve the problem if there was any.

Thank you very much for your advice. I want to try a case using the physics model of Multiphase mixture.
I met a problem here, as shown in attached figure. If I want to use only Liquid H2O, the vomume fraction of velocity inlet should be defined as [1.0, 0.0]. But I can not define it in STAR CCM. I was informed that I gave an Invalid array input.
How to solve this problem?
Would you please give me a bit more detailed information about how to set multiphase mixture model?
I am looking forward to your help.
Thank you very much!!


All times are GMT -4. The time now is 17:38.